[sisi]

I am trying to calculate the pressure coefficient of an airfoil. I googled it and found some information:

http://www.cfd-online.com/Forums/ope...s-2-2-0-a.html

Function objects are defined by additional entries in the $FOAM_CASE/system/controlDict input dictionary.

functions
{
    myFunctionObject    // user-defined name of function object entry
    {
        type                functionObjectType;
        functionObjectLibs  ("libMyFunctionObjectlib.so");
        region              defaultRegion;
        enabled             yes;
        timeStart           0;
        timeEnd             10;
        outputControl       outputTime;
        outputInterval      1;
        ...
    }
}

Example of function object specification to calculate pressure coefficient

pressureTools1
    {
        type        pressureTools;
        functionObjectLibs ("libutilityFunctionObjects.so");
        ...
        calcTotal   no;
        calcCoeff   yes;
    }

But how to modify the $FOAM_CASE/system/controlDict file? Should I add the lines to the end of the controlDict file?

functions
{
    pressureTools1
    {
        type                pressureTools;
        functionObjectLibs ("libutilityFunctionObjects.so");
        region              defaultRegion;
        enabled             yes;
        calcTotal           no;
        calcCoeff           yes;
        timeStart           10;
        timeEnd             10;
        outputControl       outputTime;
        outputInterval      1;
    }
}

Isn't working. What's wrong!?

[sisi]

I did some googeling again and found this thread. User aerothermal wrote (#3):

In Paraview is easy.

- Extract Block (the body or wing)
- Plot on Plane Intersection

So it is done!

I am obviously too stupid to understand. Please could someone give me assistance?

[alexeym]

Hi,

"Isn't working. What's wrong!?" is very uninformative. You either want people to create a case and try to check your settings to see the error you're getting (and in this case it's possible to see the answer "It's working.") or you'd like to find a) people reading the forum, b) had exactly the same problem.

It seems people found a solution in the thread you're referencing in your first message. Obviously you've tried syntax from message #20, what was the error?

[sisi]

You're right alexeym, I'm sorry

Originally Posted by alexeym

Hi,
It seems people found a solution in the thread you're referencing in your first message. Obviously you've tried syntax from message #20, what was the error?

Im getting this error when running simpleFOAM;

Create time

Create mesh for time = 0

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting RAS turbulence model SpalartAllmaras
SpalartAllmarasCoeffs
{
    sigmaNut        0.66666;
    kappa           0.41;
    Cb1             0.1355;
    Cb2             0.622;
    Cw2             0.3;
    Cw3             2;
    Cv1             7.1;
    Cv2             5;
}

    Employing Ashford correction
No finite volume options present


SIMPLE: convergence criteria
    field p     tolerance 1e-05
    field U     tolerance 1e-05
    field nuTilda     tolerance 1e-05


Starting time loop



--> FOAM FATAL ERROR: 

    request for objectRegistry defaultRegion from objectRegistry Angle-of-attack-3 failed
    available objects of type objectRegistry are
1(region0)

    From function objectRegistry::lookupObject<Type>(const word&) const
    in file ~/OpenFOAM/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 198.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::error::abort() at ??:?
#2  Foam::objectRegistry const& Foam::objectRegistry::lookupObject<Foam::objectRegistry>(Foam::word const&) const at ??:?
#3  Foam::OutputFilterFunctionObject<Foam::pressureTools>::allocateFilter() at ??:?
#4  Foam::OutputFilterFunctionObject<Foam::pressureTools>::start() at ??:?
#5  Foam::functionObjectList::read() at ??:?
#6  Foam::Time::run() const at ??:?
#7  Foam::Time::loop() at ??:?
#8  Foam::simpleControl::loop() at ??:?
#9  
 at ??:?
#10  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#11  
 at ??:?
Abgebrochen (Speicherabzug geschrieben)

Please find the attached "controlDict" file.

Also, I would like to know how to solve this problem with paraview. Is it really that easy?

[alexeym]

Hi,

about this error:

--> FOAM FATAL ERROR: 

    request for objectRegistry defaultRegion from objectRegistry Angle-of-attack-3 failed
    available objects of type objectRegistry are
1(region0)

it said you: "there's no region with a name 'defaultRegion' there's only 'region0'". Have you tried to change defaultRegion to region0?

The quote from message 3 you've mentioned in your post is actually an answer to "Also I want to plot Pressure coefficient at various positions along the length of the wing. how to do it paraview.". I.e. pressure coefficient was already calculated and person wanted to plot the values. Also because the post is from 2009, I'm not quite sure the names of the filters in paraview are the same in 2014.

In the thread you've mentioned, there is post #5, where you've got the expression for calculation of Cp. In paraview you've got Calculator filter, you can apply the filter to the whole calculation domain and then extract values from desired region. As it's simpleFoam, final solution is steady state, so you can do this paraview operation by hand and skip inventing batch process (well, you can export state from paraview as a python script and run it with slight modifications of other results; this will partly emulate batch processing with sample utility).

[sisi]

Thank you for your detailed response!

Originally Posted by alexeym

about this error:

--> FOAM FATAL ERROR: 

    request for objectRegistry defaultRegion from objectRegistry Angle-of-attack-3 failed
    available objects of type objectRegistry are
1(region0)

it said you: "there's no region with a name 'defaultRegion' there's only 'region0'". Have you tried to change defaultRegion to region0?

Yes I did, but I still have to force myself to read error messages ( "rhoInf" and "pInf" where missing). icoFOAM now works with the following settings:

functions
{
    pressureTools1
    {
        type                pressureTools;
        functionObjectLibs ("libutilityFunctionObjects.so");
        region              region0;
        enabled             yes;
        calcTotal           no;
        calcCoeff           yes;
        timeStart           10;
        timeEnd             10;
        outputControl       outputTime;
        outputInterval      1;
        rhoInf              1.225; // Air at sea level and 15 Celsius 
        pInf                101325; // Average sea-level pressure
        UInf                (26 0 0);
            
    }

"pInf" is the pressure in the freestream, isn't it? For example, on sealevel 101325 Pa. Does rhoInf=pInf=0.0 as reference values make sense? Am I using the right physical units?

How to visualize static(p)_coeff with paraview?

[alexeym]

Hi,

It's seems links from your first post were spoiled by update in docs, so here's a link to new location: http://foam.sourceforge.net/docs/cpp/a01968.html. Maybe it was vaguely written but for coefficient calculation you have to set pInf, rhoInf and UInf.

Here's a snippet from pressureTools.H

    \heading Function object usage
    \table
        Property     | Description             | Required    | Default value
        type         | type name: pressureTools| yes         |
        calcTotal    | Calculate total coefficient | yes     |
        pRef         | Reference pressure for total pressure | no | 0.0
        calcCoeff    | Calculate pressure coefficient | yes  |
        pInf         | Freestream pressure for coefficient calculation | no |
        UInf         | Freestream velocity for coefficient calculation | no |
        rhoInf       | Freestream density for coefficient calculation | no |
    \endtable

Concerning unit, by default they should be in SI, i.e. Pa for pressure, kg/m3 for density. If you take a look at pressureTools.C:

This method is called every time function object is invoked.

void Foam::pressureTools::execute()
{
    if (active_)
    {
        ...
        pResult == convertToCoeff(rhoScale(p)*p + pDyn(p) + pRef());
    }
}

p is your pressure, pResult is value that will be written to disk.

rhoScale look like:

Foam::dimensionedScalar Foam::pressureTools::rhoScale
(
    const volScalarField& p
) const
{
    if (p.dimensions() == dimPressure)
    {
        return dimensionedScalar("1", dimless,  1.0);
    }
    else
    {
        return dimensionedScalar("rhoRef", dimDensity, rhoInf_);
    }
}

I.e. if you're using solver there p is real pressure, then scale is 1, if you're using incompressible solver, where pressure is divided by density, scale is equal to the value of rhoInf.

pDyn() and pRef() are zero in your case, because you do not calculate total coefficient (I will omit code).

returning to convertToCoeff:

Foam::tmp<Foam::volScalarField> Foam::pressureTools::convertToCoeff
(
    const volScalarField& p
) const
{
    tmp<volScalarField> tCoeff(p);

    if (calcCoeff_)
    {
        tCoeff() -= dimensionedScalar("pInf", dimPressure, pInf_);

        const dimensionedScalar p0("p0", dimPressure, SMALL);
        const dimensionedVector U("U", dimVelocity, UInf_);
        const dimensionedScalar rho("rho", dimDensity, rhoInf_);

        tCoeff() /= 0.5*rho*magSqr(U) + p0;
    }

    return tCoeff;
}

This method receives pressure field in Pa, then pInf is subtracted from it, then the field is divided by 0.5*rhoInf*UInf*UInf. Guess p0 is just added to avoid division by 0 if you set rhoInf or UInf to 0.

So basically tCoeff (in your case) is just p/|UInf|^2 if I have not messed up something during code walk-though

About paraview visualization:

1. You can just use Calculator filter.

2. Pressure tools function object will write static(p)_coeff volume field for every invocation. So you just select it like you select pressure or velocity.

[sisi]

I wonder why I can't open "pressureTools.H" Link on this page...!?

An error has been encountered in accessing this page. 
...

"pressureTools.C" link is also broken!?

[alexeym]

Guess it's a "feature" of online documentation, in general there are problems with links to source files. You can always find sources in $FOAM_SRC folder. Exact location of pressure tools is $FOAM_SRC/postProcessing/functionObjects/utilities/pressureTools.

[sisi]

Originally Posted by alexeym

Guess it's a "feature" of online documentation, in general there are problems with links to source files. You can always find sources in $FOAM_SRC folder. Exact location of pressure tools is $FOAM_SRC/postProcessing/functionObjects/utilities/pressureTools.

Thanks! But I still have problems to visualize static(p)_coeff. I am looking for s.th. like that.

Step 1: $paraFOAM
Step 2: Selecting "Last Frame (500)" (Time: 500)
Step 3: Volume Fields >> static(p)_coeff
Step 4: Apply

But how to proceed? When choosing "Filter >> Calculator" I can't select anything....!? Content of "ControlDict" file is:

functions
{
    pressureTools1
    {
        type                pressureTools;
        functionObjectLibs ("libutilityFunctionObjects.so");
        region              region0;
        enabled             yes;
        calcTotal           no;
        calcCoeff           yes;
        timeStart           500;
        timeEnd             500;
        outputControl       outputTime;
        outputInterval      1;
        rhoInf                1.225; // Air at sea level and 15 Celsius 
        pInf                101325;
        UInf                (26 0 0);
            
    }
}

Is there something wrong?

[alexeym]

At this point it would be great to explain what you're trying to create in paraview, as I usually stop at point 4, obtaining color distribution. Also you either use Calculator filter on pressure volume field (to calculate pressure coefficient), or you just display static(p)_coeff (as the coefficient was already calculated using functionObject).

If you'd like to create print-quality figures from the data on airfoil, you select airfoil patch instead of internal mesh (IIRC paraview should create interpolation of pressure coefficient from internal field onto boundaries), cut it with a plain (Slice), save it as CSV file (File -> Save data) and use Matplotlib/Gnuplot/Scilab/Matlab/SomethingElse to produce PDF.

[sisi]

Originally Posted by alexeym

At this point it would be great to explain what you're trying to create in paraview, as I usually stop at point 4, obtaining color distribution.

I would like to visualize the calculated pressure coefficient static(p)_coeff. The plot should look like this. I just viewed the static(p)_coeff file. File has only one column. But I need a 2-D line plot of the data in Y versus the corresponding values in X

Originally Posted by alexeym

Also you either use Calculator filter on pressure volume field (to calculate pressure coefficient), or you just display static(p)_coeff (as the coefficient was already calculated using functionObject).

First I would like to plot static(p)_coeff. But how to manage it!?

[alexeym]

It would be rather inconvenient to plot data in paraview if you'd like to get picture similar to the one you've posted. So you should just extract values of pressure coefficient around airfoil (or just pressure) using either paraview (using Slice filter and saving data in CSV format) or using sample utility. In both cases you'll get file with 2-3 columns: (x, y, z, value) which you can plot elsewhere.

[sisi]

Ok, but I am getting strange results when plotting data using LO Calc. Just want to make sure I'm doing things right:

0. $ paraFoam
1. Last Frame
2. Mesh Parts >> airfoil - patch (only selected!)
3. Volume Fields >> p (only selected!)
4. Apply
5. Slice >> Z Normal
6. Apply
7. File >> Save Data...
8. save as *.csv
9. OK

Please find cvs FIle attached. Why do the results look so strange (data range of p)!? What am I doing wrong?

P.s.: I finally found a way to visualize cp (Pressure coefficient) with paraview (find attached cp1.png). I will post my solution tonight... I still have some questions left

[alexeym]

Hi,

As I don't see the results of your simulation, I can't say anything about pressure coefficient distribution. Can you post slice of pressure field? What BC for pressure do you have on airfoil patch?

[sisi]

@ alexeym: I followed this step by step guide. Please find attached BC and a slice (z-axis) of p. And this is how I managed to visualized pressure coefficient C_p with paraview 4.1.0:

1. $ paraFoam
2. Tool bars (time controlls) select "Last Frame"
3. Properties: Mesh Parts >> airfoil - patch
4. Properties: Volume Fields >> static(p)_coeff
5. Apply
6. Slice
7. Properties (Slice1) >> Z Normal
8. Apply
9. Select Slice1
10. Filters >> Data Analysis >> Plot Data
11. Apply
12. Display (XYChartRepresentation) >> Select Block
13. X Axis Data >> Use Data Array
14. Line Series >> static(p)_coeff (deselect all other checkboxes)
15. Line Style >> None
16. Mark Style >> Square
17. File >> Save Screenshot

So I have some questions remaining:

1. How to turn y-axis upside down in paraview!?
2. Pressure coefficient C_p at a stagnation point is usually one or less than one...!?
3. Basically, I am looking for dimensionless quantities (I will take a closer look at $FOAM_SRC/postProcessing/functionObjects/utilities/pressureTools)

Content of "ControlDict" file is

functions
{
    pressureTools1
    {
        type                pressureTools;
        functionObjectLibs ("libutilityFunctionObjects.so");
        region              region0;
        enabled             yes;
        calcTotal           no;
        calcCoeff           yes;
        timeStart           500;
        timeEnd             500;
        outputControl       outputTime;
        outputInterval      1;
        rhoInf             1.225; // Air at sea level and 15 Celsius 
        pInf                101325; // mean atmospheric pressure at mean sea level
        UInf                (26 0 0);
            
    }
}

[alexeym]

Hi,

1. In 3D view you just rotate it with mouse Or use Adjust camera button. In plot view, you press on the button "Edit view options", Left Axis -> Layout -> Specify axis range explicitly, and specify the range upside down.

2. Are you sure the case converged in 500 iterations? What are the values of residuals for pressure and velocity? In general it is better to set convergence criterium in SIMPLE dictionary in fvSolution file (see tutorials/incompressible/simpleFoam/pitzDaily for example). In general residuals around 10e-5 give good agreement with estimations/experimental values.

[sisi]

Originally Posted by alexeym

1. In 3D view you just rotate it with mouse Or use Adjust camera button. In plot view, you press on the button "Edit view options", Left Axis -> Layout -> Specify axis range explicitly, and specify the range upside down.

Thanks!

Originally Posted by alexeym

2. Are you sure the case converged in 500 iterations? What are the values of residuals for pressure and velocity?

I used the tutorial case airfoil2D (.../run/tutorials/incompressible/simpleFoam/airFoil2D) The results for 500 and 1000 Iterations are as follows:

Time = 500

smoothSolver:  Solving for Ux, Initial residual = 0.000469786, Final residual = 3.02492e-05, No Iterations 4
smoothSolver:  Solving for Uy, Initial residual = 0.000194439, Final residual = 1.46375e-05, No Iterations 4
GAMG:  Solving for p, Initial residual = 0.00255599, Final residual = 0.000166693, No Iterations 2
time step continuity errors : sum local = 3.45091e-05, global = 2.284e-15, cumulative = 5.18321e-13
smoothSolver:  Solving for nuTilda, Initial residual = 2.69677e-05, Final residual = 1.46057e-06, No Iterations 4
ExecutionTime = 36.45 s  ClockTime = 37 s

Time = 1000
smoothSolver:  Solving for Ux, Initial residual = 0.000125672, Final residual = 5.32396e-06, No Iterations 4
smoothSolver:  Solving for Uy, Initial residual = 3.1746e-05, Final residual = 1.9281e-06, No Iterations 4
GAMG:  Solving for p, Initial residual = 0.00166265, Final residual = 0.00011368, No Iterations 3
time step continuity errors : sum local = 2.34977e-05, global = 1.28775e-16, cumulative = 1.02962e-12
smoothSolver:  Solving for nuTilda, Initial residual = 7.23825e-06, Final residual = 2.52574e-07, No Iterations 4
ExecutionTime = 70.52 s  ClockTime = 71 s

But there must be something wrong with the pressure coefficient: The pressure coefficient at a stagnation point is unity or less then one. The attached screenshot shows a different result (approx -244)

[alexeym]

Hi,

as you can see residual values decreased 4 times with additional 500 iterations. So increase them even further. You can increase number of iterations (endTime) up to 25000. Solver will either converge (and stop iterating with message about convergence) or run till the endTime (in this case you've got problems with mesh, BCs, discretization).

I wasn't able to find any information about your boundary conditions. Maybe it is a problem wit interpolation of pressure coefficient onto airfoil patch. According to your pressure distribution values of pressure coefficient should be between -2 and 1 (with your Uinf = 26 m/s). Try calculate pressure coefficient in paraview using pressure distribution, rhoInf, UInf and compare it with the output of pressureTools.

[sisi]

Originally Posted by alexeym

Hi,
as you can see residual values decreased 4 times with additional 500 iterations. So increase them even further. You can increase number of iterations (endTime) up to 25000. Solver will either converge (and stop iterating with message about convergence) or run till the endTime (in this case you've got problems with mesh, BCs, discretization).

Your are right! simpleFOAM does not converge. I will check settings...